[Doginal]

Hello Everyone

I'm working to create a 2-phase model of a plate entering water, moving along a predetermined path then exiting the water while rotating independent of its motion. I have solved (after many different tests and trials as to how to get it to work) the issues of its motion/rotation by using two domain. An inside domain that contains the blade and a fine mesh which is big enough to contain the full induced flow (i.e. the inner domain is large enough that the outer domain would not be unnecessary except for the motion). Then i have an outer domain which houses the inner domain with a course mesh which is used to simply absorb the motions of the inner domain.

Everything above seems to work fine. The issue i am having involves applying a free surface. I use an unstructured tetrahedral mesh. When I apply the two-phases, i have trouble trying to solve the free surface. It seems as though because cfx is trying to solve a flat surface through an unstructured mesh, the surface keeps moving up and down as it tries to solve different iterations and timesteps. I'm not to worried about the moving surface as i'm studying the interactions between the plate and the water however the moving surface is causing velocity fluctuations and inducing currents which grow to be over 2% compared to the plate motions that i will apply.

Does any have any suggestions on what i can do to help reduce these fluctuations.

Also please note, this happens when the domain and everything stays still, as in I let the simulation run but apply no motion.

Thank You,

DM

[ghorrocks]

Can you post some images and the output file of a demonstration?

[Doginal]

Originally Posted by ghorrocks

Can you post some images and the output file of a demonstration?

Here are some pictures, I cant attach .out file because it is to large. Even when i try to zip its about 180 kb

[ghorrocks]

Then attach the CCL. It is a small text file.

Can you also do a drawing of what is going on? Where is the water level, what motion does the plate have?

[Doginal]

Originally Posted by ghorrocks

Then attach the CCL. It is a small text file.

Can you also do a drawing of what is going on? Where is the water level, what motion does the plate have?

Sorry should have at least explained it.

Finer mesh is an inner domain with an interface defined between the two domains (mesh size matches on both sides of interface).

Blade does not change position relative to inner domain.

Full inner domain will move. Path is about 1m in magnitude forward and down while the outer domain size is 30m diameter (to get you an idea of the scale of it all)

The approximate shape of path is shown in red, however as mentioned the path is much much smaller than what i penciled in relative to the size of the domains. Also the blade is about 0.5m long.

As the inner domain (and the blade with it) moves along that path there is about a 90 degree rotation applied to the full inner domain


With all that being said, in the case shown here these is no motion applied. The case i showed you everything sits still for 0.37 seconds. The velocity contours shown are completely due to free surface instability (from what i can tell at least).

The water surface level is shown by the volume fraction contour in the pictures already posted. Its the faint rainbow that goes across the domain and is about 1-2 cells thick depending on the position and if i were to post over different times, the thickness will change over time as well as it tries to solve the surface.

Hopefully i've been clear in my description, I tend to go on. Just the one important thing is that in the case shown above, there is no motion applied.

Thank You,

DM

[ghorrocks]

Please post the CCL.

Do you include surface tension?

When I did free surface modelling some time ago I set up a little test case (ie a small, simple mesh) where I tested the effects of all the free surface parameters. This allowed me to work out what was important for my model.

Free surface spreading and jiggling can be minimised by appropriate choice of time step size, convergence criteria and free surface settings. You will have to test this your self to optimise for your case.

[Doginal]

Originally Posted by ghorrocks

Please post the CCL.

Do you include surface tension?

When I did free surface modelling some time ago I set up a little test case (ie a small, simple mesh) where I tested the effects of all the free surface parameters. This allowed me to work out what was important for my model.

Free surface spreading and jiggling can be minimised by appropriate choice of time step size, convergence criteria and free surface settings. You will have to test this your self to optimise for your case.

Sorry i missed the CCL before. I just copied the first part of the output file.

I think i have played with the surface tension settings a little bit but haven't seen much of a change in the results from it. Could be that i dont really know what i'm doing with them and i'm just clicking and praying with some of those settings.

[ghorrocks]

* You are using the inhomogeneous multi phase model. Do you anticipate mixed air/water (eg fine bubble or foam)? The homogeneous model is much simpler and is more appropriate if a distinct interface exists.
* Based on the size of this model surface tension will not be significant. But surface tension puts major restrictions on the numerics so the runn will behave itself much better with surface tension off.
* Your convergence tolerance is loose. Have you checked this is OK?
* This model may work better with double preicison.

[Bfowler]

I'm a bit unsure as to how the inner domain moves, but could refining the mesh where the water surface is help? If the surface moves a lot and it's too hard to define throughout the simulation fair enough, but the CFX doc's suggest that a fine mesh at the interface could help prevent the issues you're seeing.

[Doginal]

Originally Posted by Bfowler

I'm a bit unsure as to how the inner domain moves, but could refining the mesh where the water surface is help? If the surface moves a lot and it's too hard to define throughout the simulation fair enough, but the CFX doc's suggest that a fine mesh at the interface could help prevent the issues you're seeing.

The movements really prevent localized refinement at the surface. I dont think this will really help with the issue though, the area affected seems to scale with the mesh size (like the induced flow is within x number of cells from the surface) however the magnitude of the induced flow is the same.

Refining the mesh may help to reduce area and end up helping to reduce the error but it doesn't really help the underline issues which also effect convergence.

When i've read through the cfx help it has suggested some things but seems to say this is a known issue in terms of causing propagating waves and looking to not use residuals as a convergence criteria. I'm just more taking a last ditch effort here in hopes somebody has worked through this problem before.

Re. Glen
I'll look into your suggestions. Initially i was using a homogeneous model but was having some other issues and thats when i switched to non-homo and it seemed to run better. I dont have much entrainment however I do expect some air pockets forming in the water as the plate enters. Right now however i'm more concerned with the force acting on the plate from the water and rough water interactions with the blade so slight errors with how the air pockets form as long as they dont affect the forces should not be an issue. I'll look into non-homo again.

I have tightened up my convergence criteria (max 10 iterations vs. 25) and its had no effect but i'll leave it shorter just to speed up the runs. This was something I had read about before posting which is why i tried it.

Surface tension is currently off and i'll be sure to leave it that way.

I'll try using doubler precision. I've read that before and i may have tested it a bit ago but i'll be sure to try it again.

Reading through the help documents i've tried playing with different options such as the Interface Compression Level but having seen much difference. I'm probably miss using them on account of not fully understanding but i guess i'm hoping for a magical option to fix it...don't think its out there.

Last question i guess is if you know of a way to try to separate the convergence criteria to stay away from the interface. Only thought on how to do that would involve trying to only look at area's where the volume fraction is about or below a specific number. I just dont know if something like that is possible.

The other thought to try to control the surface instabilities would be to try to create an artificial force or resistance to limit momentum transfer between the two phases. Since i'm focusing on the blade and water interaction, I dont think it should effect the results to drastically.

Once again thank you for all your help

[ghorrocks]

The choice between inhomo vs homo is more about what size bubbles you want to model. If they are big enough that the free surface model can resolve them, then go homogeneous. If you are going to get bubbles smaller than the mesh and free surface model can resolve then go inhomogenous.

By convergence I meant the convergence tolerance (currently 1e-4), not the max iterations.

Regarding the wobbling interface - this is hard to avoid in free surface models, especially in ordinary quality meshes like this. Simply put, any small wobble, even a numerical inaccuracy will cause the free surface to move and form waves whcih will propogate. This is why steady state free surface models are very tricky to converge.

[Doginal]

Thanks for the help Glenn.

I've tried both homo and non homo and both give the same effect for the free surface "wobbling"

The actual surface itself i could not care about. It really has no effect on what i'm looking at. What matters to me is the induced flow its causing.

I guess i'm just taking one last ditch effort before saying there's nothing I can do about it. I just wondering if there is any way in ansys to either solve the surface better (like using a different method to solve it) or somehow reduce the induced flow caused by the surface fluctuations. For example, a way to just dampen the flow at the surface so the surface waves a much more localized.

I know i always have the option to refine my mesh more but i'm already very close to the limits of what i can use.

[ghorrocks]

A finer mesh will probably result in more wobbles, not less.

These wobbles are very hard to reduce, especially with surface tension models. Your best bet is to improve mesh quality at the interface by putting soem high quality hex elements in that area.

You could always damp the surface region by putting a momentum sink over it but that will damp any real surface motion as well, of course.

[sjtusyc]

Glenn， I am wondering what free surface parameters did you test, and how you evaluate
whether they are important?

[ghorrocks]

What free surface parameters did I test? All of them - I systematically worked through all of them and worked out what each one did. I used a few simple benchmarks such as a drop on a surface, laplacian pressure of a spherical drop and some others and that allowed me to work out what was required for a fast and accurate free surface simulation.

But this was ages ago and I cannot remember the results. I recommend it to anybody working in this area - best to work out for yourself what works and what does not. It takes some time, but it is time well spent.

[sjtusyc]

Thank you so much.
I learnt a lo from you.
Thank you sincerely.

[Doginal]

Originally Posted by ghorrocks

You could always damp the surface region by putting a momentum sink over it but that will damp any real surface motion as well, of course.

I really dont care about surface motion at all. Even I'm worried that bubbles following the blade entering the water will produce large errors for what i'm actually looking at. For this reason I'm looking now to just eliminate all surface effects and bubble formation from the blade entering by defining the VF at all points in the domain

i.e. specify that at y>0 Volume fraction of air is 1
y<0 Volume fraction of air is 0

I just cant figure out how/where to define that. I think using a step function is the best way to define an equation for this in the same way you define the volume fraction at boundaries
step((y-UpH)/1 [m])
Where UpH is the height of the water surface (in my case 0m)
I just cant figure out where i can apply this in CFX. Like where in CFX is there an option to define the volume fraction throughout an entire domain?

Once again, any help is always appreciated

Thank You,

DM

[ghorrocks]

If you know where the free surface is and it does not move then why model the air at all? put the domain boundary on the free surface and make it an opening with a pressure of 0 Pa on the interface.

If the free surface does move but you know where it moves to you can keep it single phase by using mesh motion to make the opening follow the free surface motion.

[Doginal]

Problem is i cant make the boundary at the top of the surface due to the motion of the blade entering and moving through the water.

I need the blade to go from out of the water to in the water. The way i described above with the mesh motion is the only way i have been able to move the blade along the needed path (with the ability to make fine changes to the path) without inducing any unwanted forces. If i move the boundary to the surface, there is no way of moving the blade using the method mentioned above and I dont know of any other way to create the motion.

[ghorrocks]

What are you trying to learn with this model? What is the output from this simulation?